Learning Forum

[LPT19]

Hello!

I am currently trying to understand how static structural results are used as pre-stress input in modal/harmonic analyses, especially when it comes to stress calculation.

To do so, I created a static structural analysis with a beam clamped at one extremity, and a force (1000 kN) applied on the other extremity. The Von Mises stress distribution is just as expected, about 100 MPa (the cross section area of the beam is 100 mm x 100 mm).

Later on, I attached the results from this analysis to a modal analysis, and finally I did the same with the results from the modal analysis to a harmonic analysis, with a base excitation of 100 m/s².

However, the stress distribution of the harmonic analysis is nowhere near 100 MPa, which is the stress from the static structural analysis.

Could anyone explain to me why this happens? Shouldn't it be around 100 MPa?

Thank you in advance

Regards,

Lucas

 

[peteroznewman]

Hello Lucas,

A Static Structural solution that feeds the setup of a Modal analysis is only providing an update to the stiffness matrix of the Modal equations, which are only solved to determine the Eigenvalues (natural frequencies) and Eigenvectors (mode shapes).

Note that a Modal analysis contains no load, unlike a Static Structural analysis which requires a load.  If there is no load in a Modal analysis, there is no point in looking at the stress in a Modal analysis. The deformations in a Modal analysis are arbitrarily scaled to some norm, so the stress resulting from those arbitrarily scaled deformations is also arbitrary.

The reason to do a Prestress Static Structural before a Modal is when there is a large change in stiffness. Consider a guitar string. String it loosely into a guitar and push it sideways. It takes almost no force to push it 5 mm as the lateral stiffness of the string is very low. Tension that string till it plays a C-note.  Now it takes a very large force to push it 5 mm sideways. The lateral stiffness was dramatically increased by the tension force.

Next you have a Harmonic Response analysis. This requires both a Modal solution to feed the setup cell and a load in the Harmonic Response model.  You don't say what the first natural frequency was for the Modal solution. That is critical to know.  You used an acceleration load of 100 m/s² which has no relation to 100 MPa of stress.  You could have applied a 100 MPa pressure to the end of the beam instead of a base acceleration so you could look for that value in the results. You show the stress result at 2000 Hz, but if the first natural frequency was 20,000 Hz, that would be the reason why you have such a small result.  However, if the first natural frequency was 2000 Hz, you could have a result that is 20 times larger than the input pressure amplitude. The reason for that is resonance.  The magnitude of the response strongly depends on the structural damping ratio in the Harmonic Response analysis.

Kind regards,
Peter

[LPT19]

Hello, Peter! Thank you very much for your answer!! It really is an honor to be in contact with you!

I was just wondering if there was a way to do something similar to a solution combination, in such a way that Ansys "adds" the stresses from both static and harmonic analyses. I know it is not correct to simply add both stresses, but I wanted to see the combined effect of the force from the structural analysis and the stress generated by the harmonic analysis at a given frequency.

Thank you!

Lucas

 

[peteroznewman]

You use Solution Combination.

It's entirely valid to add the Static Structural to the Harmonic Response stress results.

[LPT19]

Hi Peter! Thank you for answering me again! Just one last question:

I am currently using Ansys 16.2 which doesn't seem to have the same functionalities as shown in your image. I am not capable of adding the results of the static structural to the results of the harmonic response (I can, however, add the results of two different static structural analyses). Is there any command to do it? I am only interested in Von Mises Stresses. Or should I add, for each element, the normal and shear stresses in all directions (x, y and z) from these two analyses, and then calculate the Von Mises stresses manually?

Thanks!

 

[peteroznewman]

Since the mesh is the same, you can output the nodal data for each component of stress for each analysis type, and add the components in a spreadsheet and compute a von Mises stress from the sum of components.